Ltspice....

[mikeks]

Folks....How on earth does one use the current controlled current source (CCCS) in LTspice....it appears not to have any control terminals....viz: no inputs for controlling current!!??!!

 

[jcx]

not obvious but you can use the attribute editor which pops up when you rt clik the f source body

clik on Value line, enter controlling Vsource name in edit line (turn on visiblity with check box)

Value2 = f source current gain

 

[mikeks]

...i need to connect the inputs (controlling terminals) of a CCCS in series with a BJT collector.....this is not at all clear in LTspice....!!?

Moreover, your figure looks suspiciously like a VCCS....not the required CCCS.....

Your thoughts?

 

[mirlo]

Put a 0V voltage source in series with the current you want to measure, and configure the CCCS (fsource) to compute its output current based on the current in that voltage source.

 

[mikeks]

i reckon i'll stick to EWB and simetrix....

 

[classd4sure]

EWB and it's latest edition multisim is brutal and there's a serious lack of selection....furthermore their free access to 100000000 parts database isn't free at all...and they force you to wait/and pay for updates by buying the latest version at full price.

Few manufacturers give Xspice models, and unless you want to make your own (learn xspice)....

What's wrong with Pspice?

Chris

 

[jcx]

sorry, thats just the way spice works, the dependent current source uses the current in a V source as input

here 0 V source V100 controls F100 without affecting collector current or Q1 operation

i also show the Behavioral Isource B1 as an alternative but behavioral sources can slow the sim

* F:\trasnsistor\Draft1.asc
Q1 N003 N002 0 0 2N2222
R1 N001 Vcoll 1K
R2 V_F100 0 1K
V1 N002 0 SINE(700m 10m 1K)
V100 Vcoll N003 0
V3 N001 0 20
F100 0 V_F100 V100 2
B1 0 V_B1 I=500*(Ic(Q1))
R3 0 V_B1 1
.model NPN NPN
.model PNP PNP
.lib F:\PROGRAM FILES\LTC\SWCADIII\lib\cmp\standard.bjt
* .op
.tran 0 2m 0 1u
.backanno
.end

 

[jcx]

lt SwCad has very good help if you already know what you're looking for, a basic SPICE book is useful, looking at the netlist and paying attention to error messages usually clears up my syntax confusions

the LtSpice group on Yahoo is really good at support and the file sharing area has many syntax/usage example files

 

[mikeks]

EWB and it's latest edition multisim is brutal and there's a serious lack of selection....furthermore their free access to 100000000 parts database isn't free at all...and they force you to wait/and pay for updates by buying the latest version at full price.

Chris

try symetrix....the free version is more flexible than multisim for analog design....download all of zetex's psice lib. from their website, and merely drag it into symetrix for totaly automated installation...

 

[classd4sure]

try symetrix....the free version is more flexible than multisim for analog design....download all of zetex's psice lib. from their website, and merely drag it into symetrix for totaly automated installation...

Ugh...multisim....I cringe at the name.

Pspice has been impressing me and I'm getting good with it..
My school actually pushed EWB as industry standard....looking back.. I can only cry.

Smart move on their part to incorporate pspice model capability.

Curious as to why you prefer it over the like of pspice but I'm willing to have a look and see for myself....so I'm ashamed to ask .....(Very)...but can you link me to their main page? As in ten minutes I've found alot of amplifiers and audio related sites....but no circuit simulators.

Thanks.
Chris

 

[mikeks]

http://www.catena.uk.com/


http://diyaudio.com/forums/showthread.php?s=&threadid=35814